[LilBort]

I am using Ansys CFX to model Displacement Ventilation in a room. I have set up and run the simulation without people in the room and with no internal heat generation. This simulation runs great and is fully functional.

Now I need to model a fully occupied room. So I created a new domain and placed it inside of the room domain, and I am using 28 cylinders to represent people in the room. I have selected this domain to be a solid domain with aluminum type solid (human skin is not an option, only aluminum, copper, steel) and an initial temp of 90 deg F. I have selected a Wall boundary type, and heat flux as the heat transfer option. But under this option the Heat Flux is labeled as Heat Flux In. So I have been using a negative value for heat flux. The people are modeled as a 5 ft tall cylinder with a radius on 1 ft. I have been assuming people give off 350 BTU/hr; therefore, I have been using a heat flux value of -.00221 BTU/(ft^2*s).

When I run the simulation I am not seeing any heat transfer into the room. Normally I would expect a natural convection plum coming off of each human body. Can someone please explain to me what I am missing? Do I need to add a boundary source, such as energy flux? Any help would be greatly appreciated. Thanks and have a great day.

[ghorrocks]

Hi,

You can generate new materials to be more representative of people rather than Al. Al, Cu, Steel are just the default pre-loaded materials. Also note that unless you are modelling heat flows inside the people you don't need to model the humans as solids. Just put the heat source on their outside walls. This way you don't need to define the material for the people anyway.

To heat the people the heat flux will need to be positive.

Have you activated buoyancy? Thermal Energy?

Glenn Horrocks

[LilBort]

I will try and run the simulation over the weekend using the energy source on the domain boundary. I will keep you updated on how it turns out.

I have activated buoyancy and thermal energy. Radiation is set to none.

[pratikmehta]

Hi,

did you set the direction of gravity in your domain

best regards
Pratik

[LilBort]

Originally Posted by pratikmehta

Hi,

did you set the direction of gravity in your domain

best regards
Pratik

In the room domain I set the direction of gravity.

In the Domain representing humans I did not. Since I chose a solid type domain for the humans, the direction of gravity is not an option.

I am trying to get a model that looks similar to this...



Where you can see natural convection plumes coming from the people

[LilBort]

I ran the model and I am still not getting the results that I want. Here are the screens shots from my simulation...





Here are the screen shots of CFX pre-processor showing the Domain and Boundary Conditions







Any suggestions?

[Mazen]

Hi Lilbort,

I am interested to model a classroom with different ventilation systems. I tried once but I faced a problem with meshing. The meshing problem arises in classroom’s tables. However, when legs of the tables were not included in the model (just the top of the tables were drawn), the meshing was ok. My question, have you tried to include tables in your geometry. If yes, would you please show me what you did?.

Regards

Mazen

[LilBort]

You should try and keep the CFD model as simple as possible. I dont think you should include tables into the model. But if you must. I would adjust the mesh size on the legs of the tables until you get a model that works. I am assuming you get an overflow error when running the simulation with table legs? If that is the case, then you should adjust the mesh size on the legs.

I saw in a different thread that you were trying to run tutorial 17. Well if you find that same tutorial in the workbench help, it explains how to build the model and mesh in Ansys Workbench. Run through the tutorial and there is a section on adjusting mesh length. Just play with the mesh size until you get a model that runs without errors.

[Mazen]

Thank you very much. I will play with the mesh size as you suggested hope it works. I forgot what the error message says.. i am not sure if it was overflow error or something else. I will try to work on it next week.

Best regards

Mazen

[ghorrocks]

Hi,

You still seem to be modelling the humans as solid bodies. Why are you doing that? It will simplify the analysis greatly if you just apply the heat flux to the outer surface of the humans. Get the basic simulation correct with the right physics before you play with mesh size.

Glenn Horrocks

[pratikmehta]

Hi,

did you run it steady or trasient , usually natural convection simulation are quite transient in nature where your time step size are very important.


Also as Glenn says it would be easier n faster if u just give heat flux to the surface of the human representation .


COuld you post your output file(.out) , in order to see if all settings are in place. I will be also better to suggest you few tips

Thanks

Pratik

[LilBort]

Originally Posted by ghorrocks

Hi,

You still seem to be modelling the humans as solid bodies. Why are you doing that? It will simplify the analysis greatly if you just apply the heat flux to the outer surface of the humans. Get the basic simulation correct with the right physics before you play with mesh size.

Glenn Horrocks

How do I apply the heat flux to outer surface of the humans without creating a domain for them? The room and human bodies are two separate meshes.

[LilBort]

Originally Posted by pratikmehta

Hi,

did you run it steady or trasient , usually natural convection simulation are quite transient in nature where your time step size are very important.


Also as Glenn says it would be easier n faster if u just give heat flux to the surface of the human representation .


COuld you post your output file(.out) , in order to see if all settings are in place. I will be also better to suggest you few tips

Thanks

Pratik

I am running a transient simulation with 1 second time steps.

Output file can be found here...

http://www.4shared.com/file/10041432..._Heat_001.html

[LilBort]

Originally Posted by ghorrocks

Hi,

You still seem to be modelling the humans as solid bodies. Why are you doing that? It will simplify the analysis greatly if you just apply the heat flux to the outer surface of the humans. Get the basic simulation correct with the right physics before you play with mesh size.

Glenn Horrocks

I took out the Human Solids Domain and added the humans into the Room Domain. Then I just created a wall boundary condition with heat flux on the human surfaces. Now the simulation gives me a isolated fluids region error. How do I set the pressure inside the human regions in order to avoid this error?

[ghorrocks]

Hi,

You don't need to model the humans at all. Delete the domains containing the humans. Place a heat flux on the outer surface of the humans to model the effect.

Had a quick look at your output file:
* You HTC on all walls is very small. Why did you use such a small number?
* You should specify either the inlet or outlet as a pressure boundary. Read the documentation for more information about how to specify BCs.
* Monte Carlo radiation is very expensive. Consider the Discrete Transfer radiation model, or no radiation model if it is not significant.
* Max no of coeff loops=3 is very small. This should be at least 10.
* Why use mem allocation factor =5? Unless you need it then don't set it.
* Consider using adaptive timesteps.

Glenn Horrocks

[LilBort]

Originally Posted by ghorrocks

Hi,

You don't need to model the humans at all. Delete the domains containing the humans. Place a heat flux on the outer surface of the humans to model the effect.

Had a quick look at your output file:
* You HTC on all walls is very small. Why did you use such a small number?
* You should specify either the inlet or outlet as a pressure boundary. Read the documentation for more information about how to specify BCs.
* Monte Carlo radiation is very expensive. Consider the Discrete Transfer radiation model, or no radiation model if it is not significant.
* Max no of coeff loops=3 is very small. This should be at least 10.
* Why use mem allocation factor =5? Unless you need it then don't set it.
* Consider using adaptive timesteps.

Glenn Horrocks

- I noticed the HTC were in the wrong units, I have since changed them to English units.

- The inlets and outlets have fixed velocities, and the room should pressurize.

- I am considering turning radiation off all together. I was using radiation through the windows, but radiation takes so long to heat objects up, and my model is only running for 15 minutes.

- Once I get my model to run correctly I will increase the number of loops.

- I increased the memory allocation because I was getting overflow errors.

Now I think I have almost got it. I delete the domains containing the humans and place a heat flux on the outer surface of the humans. Now I am getting the isolated fluid regions error, but I think my model is set correctly. How do you turn the isolated fluid regions check off? I cannot find where to edit expert solver parameters.

[rikio]

For the isolated regions error, I think domains of humans are included in your model, right? This error comes out when separated & closed domains included. Just dig meshes for humans from the domain of room, and set the cylinder faces as outer surface of humans. Saying, edit your mesh file again.

[ghorrocks]

Hi,

"The inlets and outlets have fixed velocities, and the room should pressurize." - this sounds like rubbish to me. The room will just keep increasing in pressure as time progresses. If you want to want to pressurize the room you need to specify the inlet and outlet flow curve and any leakage paths. Then the room will naturally find its pressure level between the inlet and outlet.

"I am considering turning radiation off all together" - work out the radiation heat fluxes. If they are insignificant compared to the convection and conduction fluxes then yes, turn them off.

"Once I get my model to run correctly I will increase the number of loops" - this is not a good way of quickly getting a starting point. You need the timesteps to come close to converging or you can get very misleading results. Use a max coeff loops of 10 or more right from the start.

"I increased the memory allocation because I was getting overflow errors" - then fix the overflow errors. This shows there is something seriously wrong with your model and you only been lucky that increasing memory allocation allowed it to continue. I doubt the results are sensible, you could get anything.

Glenn Horrocks

Glenn Horrocks

[Simulation Engineer]

Hi - a couple of thoughts and maybe you already have these:

Did you set up Domain Interfaces of solid - fluid type between all the solid cylinders and air in the room?

did you use buoyancy and set gravity vector direction and ref density for fluid?

did you use Air Ideal gas model for air if it is natural convection?

[LilBort]

Originally Posted by rikio

For the isolated regions error, I think domains of humans are included in your model, right? This error comes out when separated & closed domains included. Just dig meshes for humans from the domain of room, and set the cylinder faces as outer surface of humans. Saying, edit your mesh file again.

I am going to look into this. I will redo my mesh such that it is all contained in one domain. So I will not have a humans domain, just cylindrical indents in the floor of the room. And I will set a heat flux on the cylinder surfaces.